I think i am almost ready to send this in to be made, but I wanted to just have someone go over it first seeing as how it is my first time.
Couple of questions: Is it OK to have the silkscreen go on top of traces? I’m assuming that it doesn’t interfere at all.
You’ll notice that the four voltage regulators in the middle of the board have custom footprints that I created myself, to go along with the following heatsink:
One thing that I notice now, is that the base of this heatsink is metal and will be sitting directly on the board. But the board has traces that run right through the heatsink so they will be touching… How do i avoid this ? (The heatsink is connected to the GND pin of the voltage regulator in most cases)
Re the heatsinks - the tracks running under them would be better off on the other side if the heatsink touches the laminate.
OR simply do not run them under the heatsinks - there is plenty of room not to.
If the regulators need heatsinks how much current is being drawn?
Consider the track widths of your AC input and into the regulators. it may be too thin.
The crystal needs to be next to the pins it connects to not the other side of the board.
The diodes/bridge would be better off over near the input pins, what about a reservoir cap and a fuse?
I cant quite see where all the other side tracks are supposed to go - can you post the file & schematic?
Should the caps be where they are or perhaps around the IC?
It’s twice the size it needs to be - does it need to be so large for so little?
The caps say they are 100uf and 1000uf but are small like they are only 1uf mono sized.
Are you sure you have the correct footprint? and their placement is IMO too far away from where they should be working.
Some of those track lengths are very long from out of the IC - should they really be that long - are the external connection pads in fixed positions that cannot be closer to the IC?
I would consider ripping it up and starting again. soz.
mattylad:
Re the heatsinks - the tracks running under them would be better off on the other side if the heatsink touches the laminate.
OR simply do not run them under the heatsinks - there is plenty of room not to.
OK, will run them under the heatsinks. I just used the autorouter for everything BTW- is there a way to prevent the autorouter from using that area?
mattylad:
If the regulators need heatsinks how much current is being drawn?
Consider the track widths of your AC input and into the regulators. it may be too thin.
Could be up to 1.5 amps of current. I will manually route those tracks and make them a bit bigger.
mattylad:
The crystal needs to be next to the pins it connects to not the other side of the board.
The diodes/bridge would be better off over near the input pins, what about a reservoir cap and a fuse?
I cant quite see where all the other side tracks are supposed to go - can you post the file & schematic?
Should the caps be where they are or perhaps around the IC?
Ok, it shouldn’t be a problem moving the crystal to the other side of the board. There is a fuse built into the case(along with the step down transformer).
mattylad:
It’s twice the size it needs to be - does it need to be so large for so little?
The caps say they are 100uf and 1000uf but are small like they are only 1uf mono sized.
Are you sure you have the correct footprint? and their placement is IMO too far away from where they should be working.
Some of those track lengths are very long from out of the IC - should they really be that long - are the external connection pads in fixed positions that cannot be closer to the IC?
I would consider ripping it up and starting again. soz.
The physical dimensions of the board match my pre-made case w/ mounting holes exactly… Caps C1-C4 are actually 1800uF each, and are huge. thats why i tried to space them out as much as possible. I guess the footprint is wrong; I will try and find one that matches my caps a bit better.
Thanks again for the input, and ill post another board here in a couple hours along with the schematics.
-One thing i noticed is that there are a couple of VIA’s that don’t seem to have any connection on them, yet i can’t remove them. Weird.
-I also just thought of something that could possibly pose a big problem: When i designed the package for my clip on heatsinks, I barely left any room at all between the three green pads. Does this mean that they will be electrically connected?
sk_uk:
The track from pin 9 of the Atmega328 going to C9 looks like it crossed the +5v.
You should run the DRC check, it will pick this up.
Move the crystal and the two caps a bit more closer to the Atmega328 and make it symmetrical.
Yep- it was crossed. Thanks for pointing that out. Ran the DRC and it also indicates problems with my heatsink package, so i will have to fix that as well. It also lists many clearance errors and drill size errors. Looks like there is still work to be done.
BTW, i’ve never used the DRC check before. I just hit it without changing any of the settings. I’m assuming that’s okay?
I’d suggest, for the sakes of avoiding picking the wrong package, print out your PCB layout to a printer, and then physically check that all the parts will fit (assuming you actually have the parts on-hand). That will avoid issues with picking the wrong package for the ATmega328, and oversized capacitor packages and stuff.
The 7915 is NOT an inverting supply, it is only a negative regulator. You CAN NOT generate a -15v supply that way.
The 78xx/79xx regulators need ceramic caps near their pins to prevent oscillations. Check the data sheets; I would put 100n on the output of each and 100n or 330n on the input. These should be right at the pins of the regulators.
I would add an ISP header to allow programming withour removing the processor from the board
The wiring of R5 and the contrast pin of the LCD is wrong. Use a 10k pot, one end to +5, the other to ground, and the wiper to contrast. If the adjustment is too crowded on the low end, put a resistor between +5 and the top of the pot.
Does the LCD need a current-limiting resistor for the backlight? Many do. If so, add it between pin 15 and +5
Look into using either a 16 pin single-row or 2x8 pin header for the LCD; it will make wiring easier.
In schematics, it is conventional to have positive voltages point up, ground and negatives down.
I would add another 100n bypass cap for the ATMega; place one right by pins 7/8 amd the other by 20/22
Since you are using the ADC, put a 100n cap between pin 21 and ground to bypass the on-chip reference. You will need voltage dividers for the other rails. Note that the ADC can’t measure a negative voltage; the common trick here is to set up a voltage divider between the negative rail and +5 instead of ground to offset the voltage to the positive side
R1 is usually 120R or 240R; verify that 47R is really what you want
I would add a resistor from the 317’s adjust pin to ground (in parallel with the pot). As it is now, if the pot gets disconnected, you will see the full DC rail on the 317’s output.
How much current will you be drawing from the +5 rail? Since your DC bus will have to be at least 22V (15V plus 7V headroom), the 7805 will get quite hot dropping 17V.
Previous designs used a ground plane; the latest doesn’t. I would use the ground plane; if you don’t want to, at least tie the copper pour to ground to reduce noise. Try to minimize the number of traces on the side with the ground plane so it doesn’t get cut into Swiss cheese.
Traces should exit pads straight out, not at angles; traces connecting pads or other traces, or even bending at acute angles can cause acid traps during etching.
I would label the connection pads with their purpose; it will make bringup easier. Also add the board name and version or date to the silk. Put an extra ground pad next to each power supply output and the pot’s pad.
You might want more mounting holes by the heatsinks to avoid having the board flex.
Wow, that looks like lots of things to change. Thanks for the reply.
n1ist:
A few issues:
The 7915 is NOT an inverting supply, it is only a negative regulator. You CAN NOT generate a -15v supply that way.
How should it be connected? I've connected it similarly on a breadboard and it is working.
n1ist:
The 78xx/79xx regulators need ceramic caps near their pins to prevent oscillations. Check the data sheets; I would put 100n on the output of each and 100n or 330n on the input. These should be right at the pins of the regulators.
I will add one more cap to the output of the 7915, and move the other caps closer.
n1ist:
I would add an ISP header to allow programming withour removing the processor from the board
The wiring of R5 and the contrast pin of the LCD is wrong. Use a 10k pot, one end to +5, the other to ground, and the wiper to contrast. If the adjustment is too crowded on the low end, put a resistor between +5 and the top of the pot.
I'll think about the ISP header, but it is optional for me as I have no issues with removing the board.
As for the contrast pin, i’ve hooked this entire circuit up on a breadboard and found that 2k ohms works best.
n1ist:
Does the LCD need a current-limiting resistor for the backlight? Many do. If so, add it between pin 15 and +5
Ill check the datasheet. I noticed that the voltage regulator got piping hot when my backlight was on- the initial reason as to why i included heatsinks. Ill check this out.
n1ist:
Look into using either a 16 pin single-row or 2x8 pin header for the LCD; it will make wiring easier.
Yeah, i’ve thought about that because there will be a lot of wires to solder to the board as is. I really have no idea what type of connectors to use- i’ve looked through digikey but just get lost…
n1ist:
In schematics, it is conventional to have positive voltages point up, ground and negatives down.
I would add another 100n bypass cap for the ATMega; place one right by pins 7/8 amd the other by 20/22
Since you are using the ADC, put a 100n cap between pin 21 and ground to bypass the on-chip reference. You will need voltage dividers for the other rails. Note that the ADC can’t measure a negative voltage; the common trick here is to set up a voltage divider between the negative rail and +5 instead of ground to offset the voltage to the positive side
Will do. I’m only measuring the +Vadj from LM317, as the other voltages don’t change and I know their values.
n1ist:
R1 is usually 120R or 240R; verify that 47R is really what you want
I would add a resistor from the 317’s adjust pin to ground (in parallel with the pot). As it is now, if the pot gets disconnected, you will see the full DC rail on the 317’s output.
Will do- 47 works for me in this situation.
n1ist:
How much current will you be drawing from the +5 rail? Since your DC bus will have to be at least 22V (15V plus 7V headroom), the 7805 will get quite hot dropping 17V.
Yeah, i’m hoping the heatsinks will do a good job of disappating it. Theoretically I suppose it could go up to 1-1.5 amps, but I doubt that will ever happen.
n1ist:
Previous designs used a ground plane; the latest doesn’t. I would use the ground plane; if you don’t want to, at least tie the copper pour to ground to reduce noise. Try to minimize the number of traces on the side with the ground plane so it doesn’t get cut into Swiss cheese.
Traces should exit pads straight out, not at angles; traces connecting pads or other traces, or even bending at acute angles can cause acid traps during etching.
I would label the connection pads with their purpose; it will make bringup easier. Also add the board name and version or date to the silk. Put an extra ground pad next to each power supply output and the pot’s pad.
You might want more mounting holes by the heatsinks to avoid having the board flex.
/mike
Great advice… thanks a lot. Really appreciate it all, as a complete newbie to this stuff. The ground plane is in fact there in the other pictures- i left it out in one picture to make the traces easier to see. I put a ground plane on both sides… is this not a good idea?
As for labelling and silkscreen I have yet to do that, but everything that needs to will be getting a label.
I missed the separate “ground for -15V” in the schematic. The 7915 (with bypass caps) will work in the current circuit, however you can
NOT tie the "ground for -15V) pin to the main ground as it will short out the DC bus. It can’t be used, for example, to make a +/-15V supply for an op-amp. A better way would be to either use a center-tapped transformer (or second one) to create a true split supply, or use an inverting or isolated DC/DC converter.
The problem with the LCD contrast is likely a schematic error. As wired, the 2K resistor is just between Vcc and GND.
As for going to 1-1.5A, there are two problems with that. Your bridge is only using 1A diodes (and that’s a max current spec). Also, at that current, the regulators will shut down due to overtemperature. The 15V regulator is dumping 7V into heat, and the 5V regulator is dumping 17V. 17V drop at 1A is 17W, way too much for that package and heatsink.
Right now, you have a copper pour on both sides of the board, but it isn’t tied to ground, so it isn’t a ground plane. Your previous board (pictures from 9/7) are better from a grounding point of view.
I’m guessing you are trying to make a bench supply here. What I would do is take two transformers, one center tapped one for the +/-15 and adjustable regulator, and one for the 5V one. That will give you all three voltages referenced to the same ground. Pick the voltages to minimize heating in the regulators.
